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There's no simple, one line answer, so this might be a long reply. Basically, I have Design Expert and love it.
But I started with Atom, and hated it.
Some of my observations regarding Alibre, and the former Inventor/Solidworks/ Fusion users who come over to Alibre Forum with questions while trying the Alibre products.
Alibre has three levels of CAD. The hobby level Atom, then the other two (Pro and Expert).
Atom is very different from Pro and Expert. It's barebones, modeling and drawings. Nothing else.
1. First, I'll talk about Atom.
Atom is very capable, but there are no "easy buttons". If your coming from Fusion, you'll probably expect lots and lots of easy buttons, and get really frustrated that they don't exist. By "easy buttons", I mean things the average Fusion user will take as normal, indespensable, like a thread button, a scale button for changing the size of a sketch, etc, etc. In Atom, everything will be done the hard way.
Example of creating threads the hard way, with no thread button in Atom:
In Atom, all of the things your accustomed to doing with a single click in Solidworks/Inventor, will be done the hard way. To scale up a sketch, you'll constrain and dimension the various lines, arcs, etc, until it's the right size.
The good part about Atom,l is that it is the world's best training tool for Design and Expert. IF you have the patience and persistence to become competent with Atom, you'll be able to accomplish anything with Design/Expert.
2. Now Design/Expert
They are pretty much the same CAD (solid modeling and drawings) program. Expert comes with a sheet metal module and a very good third party program, Keyshot, for rendering photorealistic images, whereas Pro is basically just the modeling and drawings modules.
Pro and Expert have most, if not all, of the easy buttons that an Inventor/Solidworks user would be accustomed to.
All of Alibre's CAD versions work similar to Solidworks, but with a kinda, backwards workflow. Alibre likes simpler sketches, preferring the complexities to be done in the 3d modeling environment.
Example: in Solidworks, to create a cube with filleted edges, I would create a square sketch, then fillet the corners of the sketch into a cube. In Alibre, it better handles it with the sketch left square, and the fillets added to the solid part after.
Alibre prefers more, simple sketches. No overlaps allowed. Only closed loops. whereas an Inventor user can create a complex sketch, then choose various parts of the sketch to extrude in different ways. In Alibre, it's simple sketch/ extrude. Then another simple sketch/extrude, etc. basically, accomplishing the same thing in a linear manner, via lots of small steps, instead of all at once.
Another example:
In Inventor I might create a motorcycle clutch cover by sketching the exterior perimeter. Then sketching the interior cavity then sketching the screw pattern. All in one sketch. After, I'd do an extrude operation on the outer perimeter to 25mm thick (create the body), select the inner sketch and extrude to only 5 mm thick, (the cavity), the select the screw holes and extrude cut "through all" to leave the holes.
Whereas in Alibre, to get the same part I'd first sketch the outer perimeter, and "extrude boss" it into a solid. Then I'd sketch the cavity and "extrude cut" to the needed depth. Then, is sketch the screw pattern and "extrude cut" all the way through.
So, basically, in Inventor you can do one big complex sketch, then one big complex extrude.
With Alibre you'll need to do simple sketch/extrude, sketch/extrude, sketch l/extrude.
Hope this helps
